Creating a new Part on the curve surface in Assembly-Autodesk Inventor 2013 (with caption and audio)

Serial No. 194

Creating a new Part on the curve surface in Assembly-Autodesk Inventor 2013 (with caption and audio)

In this exercise, a pre constructed part file (Base) is utilized, which is taken from our model ‘Can’.

 

Click the following link to get the model file: - http://bit.ly/2nO8BeB

 

 

Transcription of Video

We have following cylindrical component named ‘Base’ in our incomplete assembly.

The target is to create and fix a ‘Clip’ on its cylindrical face.

1. Now create a new component in the assembly with the name ‘Clip’.
2. Select the Standard (in).ipt template for the new part file.
3. Select the Centre point of the assembly as a base plane for the new component.
4. Return back to the assembly environment by clicking Return icon.
5. At present the part is not fully constrained in the assembly.
6. Remove the degrees of freedom of the component (Clip) by applying Mate constraints.
7. So, after applying the Mate constraints no degrees of freedom is left in the Assembly.
8. Double click the Clip part to edit it.
9. Create a new sketch on the XY Plane of the Clip.
10. Take the project of base part with the help of Project Cut Edges tool.
11. Convert all the sketches into construction geometry.
12. Exit the sketching environment.
13. Create a new Work Plane on this point, perpendicular to projected vertical line of the base part.
14. Create a new sketch on this work plane.
15. Take the project of base part once again.
16. Exit the sketching mode and change the name of the sketch as ‘Base sketch of Clip’ in the Browser Bar.
17. Again enter in the sketching environment.
18. Draw the desired sketch with the aid of 2D sketching tools as displayed.
19. Use the constraints to properly position the sketch.
20. Convert unwanted sketches into construction geometry.
21. Now our base sketch is complete.
22. Finish the sketch and start a new sketch on the same work plane.
23. Take the project of following intersection points and arcs of the sketch.
24. Close the visibility of the base sketch to see the projected points and arcs clearly.
25. Complete the sketch as displayed.
26. Now our sketch is complete so exit the sketching environment.
27. Extrude this sketch profile 5/8 inch in the downward direction.
28. Change the colour of the Part to ‘Steel’.
29. Return back to the assembly environment.
30. Check the interference between the both parts with the help of ‘Analyze Interference’ tool that is available on the Interference panel of Inspect tab.
31. Activate the tool, first select the Base part and then the Clip, click Ok to Analyze.
32. There was no interference detected.
33. Edit the Clip part once again.
34. Create a new sketch on the front face of the Clip.
35. And draw sketch profile as displayed.
36. Extrude the sketch profile and select Cut option in the extrude dialog box.
37. In the Extents field select ‘All’ from the drop down list to remove the material from the Clip.
38. Mirror this extrude feature with the aid of Mirror tool.
39. Select XY Plane of the Clip as mirroring plane.
40. Now create a hole on the front face of the Clip.
41. Hole should lie on centre of the front face.
42. Now our model is complete.